chamfering with a spot drill

[mielke]

Does anyone have any advice? I have 1/2" holes and want to put a little chamfer on them. The material is 304 SS and i have a 1/2" hss spot drill. I was thinking of just using the spot drill to interperlate a chamfer on the hole. the recommended speeds and feeds for the spot drill are very slow and would take forever to chamfer all my holes. I am thinking that the speeds and feeds i have are for spot drill (actually drilling a hole in the material) but since i am only nicking the edge to produce a chamfer I should be able to go alot faster but cannot find any references on speeds and feeds. I could experiment but i realy dont' want to wear down the spot drill.

 

[MikeHalloran]

You need to buy a bigger spot drill, or an actual countersink.

You could orbit a 1/2" spot drill around the edge of a 1/2" hole, but it will take a while, and you'll want to curl the beginning and end, sort of like they do with thread milling.



Mike Halloran
Pembroke Pines, FL, USA

 

[MikeHalloran]

Also, you need to make the orbit go slow, unless you want a scalloped chamfer.


Mike Halloran
Pembroke Pines, FL, USA

 

[mrainey]

If you have a lot of holes to do, you might consider something like a Cham-Bit.

http://www.vernondevices.com/chambit.htm

Software For Metalworking

http://closetolerancesoftware.com

 

[ornerynorsk]

Your speeds and feeds will not change just because you "are only nicking the edge". Can you afford the extra time of a tool change to do it properly, or use a larger spotting drill as suggested by Mike?

 

[ProgressiveRacing]

Actually, YES, you can run the tool at a speed suitable to your effective diameter. For instance, Z-.100 (for interpolation) @ 90º included, is a .200" diameter milling tool. SFM should be set to that tool diameter, not a 1/2" drill. Being a light peripheral cut, sfm can be on the higher side without an issue.



The Manufacturing Reliquary

http://cmailco.wordpress.com/

 

[ornerynorsk]

My point was that you cannot exceed your normal speed for a given diameter just because of the small amount of material being removed.

 

[saberblue]

Why not get a larger spot drill and use it as a spot drill but take it deep enough to chamfer the hole before you drill it -- the spot drill will give you better location and less drill walking -- just a thought

 

[BrianE22]

What size hole are you drilling? Like Saberblue says, there may be a bigger spot drill that would give you the chamfer. You can also have a tool grinder make a special spot drill to both drill and chamfer.

 

[ProgressiveRacing]

Short of employing a cham-bit, as Mike suggested, or using a custom tool, saber's suggestion is your best bet; use a larger spotter.

ornery,
My point is that you can. The reason the sfm suggestion is there in the first place is due to the tool's ability to withstand heat; that is not only determined by the tool & workpiece material, but the amount of tool engagement. Adequate chip/tooth and low radial engagement means less heat in the cutting tool, which leads to higher sfm and more productive feed rates.

The Manufacturing Reliquary

http://cmailco.wordpress.com/

 

[ornerynorsk]

Hi Progressive,

There are some materials and tooling that you can get away with doing that. Not HSS tools on 304 SS. You will get a very concentrated localized heat build up on the tool as soon as your excess velocity has knocked the keen edge off and you'll end up with a nice groove in the tool in very short order, even if you're only producing a .010 chamfer running coolant or an evaporative fluid.

I've done more than a fair share of 304 stainless in my (way too many) years in the shop, and I can tell you this as fact from practical experience, not what is contained as theory in sales literature. I've literally melted the business end off of endmills (with coolant) trying to cheat feeds and speeds, where in the opposite side of the coin, I've done dry milling using sane speeds with nary a browned chip. Velocity is a major factor to tool life as the material becomes tougher and more abrasive.

 

[saberblue]

Have not done a lot of 304 but lots of 3/8 16 holes 3/4 deep in 316L testing the efficiency of metal working fluids (spot drill/chamfer, drill, ream and tap)- with out any problems- if you have problems with chip welding wipe on a little heavy high viscosity tapping compound or paste on the
tool and or put a spot on where you are going to spot drill and drill thru it

 

[ProgressiveRacing]

Hi ornery,

I can't say that I've had the same experiences. One of my clients builds custom equipment for optometry from time to time, much of which is comprised of 304L componentry. The first programs I worked out for them, I suggested moving away from the numerous M42 HSS chamfer mills they'd made from unfortunate end mills. Understandably so, they wanted to consume the stock on hand, and so I set out programming all of the chamfers (.050) with the M42 HSS cutters in mind. I wrote those programs employing effective diameter compensation and respective sfm, just as outlined earlier. Chip/tooth was set to .0015 and nary an issue with the tools, though I am sure they needed regular replacing. I was there for the first batch runs and did not notice any abnormal wear on the cutters, though I pitched using the Iscar-type screw-on cham-mills for future lots. YMMV.

Regards,
Chuck

The Manufacturing Reliquary

http://cmailco.wordpress.com/

 

[MikeHalloran]

Let me propose something, for purposes of argument.

This is _way_ beyond my programming ability, but I think that on _some_ machines I have seen, it should be possible. As a minimum, you'd need a machine that's capable of rigid tapping, i.e. with a spindle that can run smoothly at very slow speed. You'd also need the ability to orient the spindle to a particular orientation, and you'd have to set up the spotting drill both for depth and for angular orientation relative to the spindle key.

In summary, you would, for chamfering a 1/2" hole with a 1/2" spotting drill:

- Orient the spindle so one cutting edge is radial to the hole.
- Translate along that direction so that one cutting edge now touches the edge of the hole, or will, with a little axial feed.
- Start the spindle at, say, 10 rpm, and at the same time, start orbiting the hole, also at 10 rpm, in the same direction.
That keeps the single cutting edge radially aligned to the local hole edge.
Feed axially to make the chamfer while orbiting and rotating at the same time, pulling a single chip just like a machinist does with a deburring tool.
Withdraw axially to stop cutting, then stop the orbit and the rotation, or just go to the next hole.

NOTE: I HAVE NEVER SEEN THIS DONE.
I'm just thinking it SHOULD be possible on at least some mills.
Of course, if you get it wrong, and the spindle doesn't rotate and orbit in exact synchronization, or the drill edge doesn't start out in the exactly correct angular position, you just rub the edge off the tool and make a mess.


Mike Halloran
Pembroke Pines, FL, USA

 

[ornerynorsk]

Good suggestion Mike. I've never done this on anything except a straight edge with the spindle off. Basically shaping or broaching. Honestly, I don't know that it's possible on ~most~ cnc machines to run rigid tap that slowly and to simultaneously run a mill bore canned cycle or to even move the x or y axis with a rigid tap in effect. Might be worth checking out as it would speed the process up tremendously.